[diamondx]

Hi everyone,
I just started a new job when I will have to deal with CFX. I come from Fluent, and I was wondering what is the equivalent of the under relaxation factors in CFX, and where to change them. Are there any best practice to relax and help converge a solution. Any link will be aprecciated, thanks a lot

[diamondx]

Okay it looks like I found them in the expert paramaters -> convergence control -> relaxation parameter. I guess there is no way to change this for each variable, like pressure, turbulent viscosity...

[JuPa]

Don't mess around with expert parameters.

Under relaxation factor in Fluent = physical time step in CFX.

High physical time step advances the flow fields but may cause instabilities.
Low physical time step doesn't advance the flow fields as much but will cause less instabilities.

As you advance toward a converged steady state solution you can increase the physical timestep.

You can change the physical timesteps on the fly whilst a simulation is running.

Read the CFX guide.


Welcome to CFX.

[diamondx]

Thanks for you answer, by timestep you mean fluid timescale control in the solver control tab ??

[Opaque]

Correct, or Solid Timescale Control in case with solids.

[diamondx]

Thanks, another question, I'm trying to monitor my velocity at the oulet. So i created a new monitor in the monitor output. Since I am using a cluster, I would like to be able to view it listed with my residual. I can not see it. Is there an option to choose between plot and print to console ?

[ghorrocks]

You can see graphs of all these parameters in the solver manager. You can also export the raw numbers.

[diamondx]

@glenn thanks, it's not what I want. I use a cluster, I can't interact with it while it's solving, I want it to print my monitored point with the residuals at every iteration. Or may be it not possible ?

[ghorrocks]

The solver manager works on clusters as well as local machines.

[singer1812]

Diamond you just open Solver Manager>>Monitor Run In Progress

Navigate to your run directory, and choose the .dir directory that is your current run.

Solver manager will open up and monitor that job, with the residual and monitor point graphs displayed.

[Opaque]

To complement Glenn's and Singer's responses:

The ANSYS CFX Solver Manager is an independent application from the ANSYS CFX Solver. It can monitor a calculation in progress if it can read the "running directory" for the given calculation. The calculation may be done on a different computer (or operating) system, and it still can monitor the calculation as long as it has read permission of the folder/directory and the files within it.

Also, have you looked at the command line utility cfx5mondata? This utility allows you to extract data from a given finished/running calculation. You can do cfx5mondata -help for additional information.

Hope the above helps,